Cd too high with k-w SST

giammy92 · April 21, 2016, 13:34

Dear all,
I'm performing a thesis in which i have to calculated force coefficients of an airfoil 2 D invested by a flux inclined of 13 deg compared to chord. I want use k-w SST and simpleFoam. I report you my 0 file:

-K

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.0025847;

boundaryField
{
TRAILING_EDGE
{
type fixedValue;
value uniform 1e-12;
}
SUCTION_SIDE
{
type fixedValue;
value uniform 1e-12;
}
FAR_FIELD
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.001;
value uniform 0.0025847;
}
PRESSURE_SIDE
{
type fixedValue;
value uniform 1e-12;
}
frontAndBackPlanes
{
type empty;
}
}

-NUT

dimensions [0 2 -1 0 0 0 0];

internalField uniform 1.4599e-6;

boundaryField
{
TRAILING_EDGE
{
type nutLowReWallFunction;
value uniform 0;
}
SUCTION_SIDE
{
type nutLowReWallFunction;
value uniform 0;
}
FAR_FIELD
{
type calculated;
value uniform 1.4599e-6;
}
PRESSURE_SIDE
{
type nutLowReWallFunction;
value uniform 0;
}
frontAndBackPlanes
{
type empty;
}
}

-OMEGA

dimensions [0 0 -1 0 0 0 0];
internalField uniform 1770.43;

boundaryField
{
TRAILING_EDGE
{
type fixedValue;
value uniform 1e-12;
}
SUCTION_SIDE
{
type fixedValue;
value uniform 1e-12;
}
FAR_FIELD
{
type turbulentMixingLengthFrequencyInlet;
mixingLength 5.2428e-5;
value uniform 1770.43;
}
PRESSURE_SIDE
{
type fixedValue;
value uniform 1e-12;
}
frontAndBack
{
type empty;
}
}

-P

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
TRAILING_EDGE
{
type zeroGradient;
}
SUCTION_SIDE
{
type zeroGradient;
}
FAR_FIELD
{
type freestreamPressure;
}
PRESSURE_SIDE
{
type zeroGradient;
}
frontAndBackPlanes
{
type empty;
}
}

-U

dimensions [0 1 -1 0 0 0 0];

internalField uniform (40.447 9.338 0); // (41.511*cos13 41.511*sin13)

boundaryField
{
TRAILING_EDGE
{
type fixedValue;
value uniform (0 0 0);
}
SUCTION_SIDE
{
type fixedValue;
value uniform (0 0 0);
}
FAR_FIELD
{
type freestream;
freestreamValue uniform (40.447 9.338 0);
}
PRESSURE_SIDE
{
type fixedValue;
value uniform (0 0 0);
}
frontAndBackPlanes
{
type empty;
}
}

My mesh is enogh refine to wall, i have y+ about 1 or less, so i don't use wall function and I've used for k, omega and nut the bc suggested for a mesh with y+<5, by this site http://www.dicat.unige.it/guerrero/o...turbulence.pdf

I've achieved an acceptable value of Cl of about 1.17 against 1.2 of experimental data, but my Cd is far away, 0.07 against about 0.02 of exp. data.

My supervisor suggests me to change wall's bc for k and omega without use wall functions...but i don't have any idea of which kind of bc i can use

Do you recommend me change other bc?

Please help me, this problem is taking me a long time, I want graduate quicky!!!

giammy92 · April 21, 2016, 13:47

fv Schemes

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
div(phi,U) bounded Gauss GammaV 0.2;
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,omega) bounded Gauss limitedLinear 1;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

fv Solution

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 1;
tolerance 1e-08;
relTol 0;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

}

SIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;

residualControl
{
p 1e-5;
U 1e-5;
k 1e-5;
omega 1e-5;
}
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
omega 0.7;
}
}

Kina · April 22, 2016, 03:54

Do you know from your physical conditions that the boundary layer is fully turbulent?
kOmegaSST in OF models fully turbulent conditions. Maybe you have to implement a transition model. Also, try to change your scheme for div(phi,U) as it affects the drag value by a large percentage. For my problem, drag reduces by more than 10% with "bounded linear" instead of "bounded linearUpwindV grad(U)".

Cheers
Alex

giammy92 · April 22, 2016, 06:38

thank you for your reply Kina

Yes my boundary layer is fully devoleped, i have Re = 1.5 e6.
Furthermore my supervisor suggests me to try with calculated k and omega to wall. Is it reasonable?

Kina · April 22, 2016, 07:13

Your omega values are kinda weird. I suggest you calculate your omega with the second omega equation given here: http://www.cfd-online.com/Wiki/Turbu...ary_conditions

set your omega to 10^8 at walls. yours is too small as omega theoretically rises to infinity at walls.

Cheers
Alex

giammy92 · April 22, 2016, 07:45

but which type of bc for omega?
fixedValue or calculated?

Kina · April 22, 2016, 08:28

fixedValue. I wouldn't set k or omega to calculated - I am not even sure if that's possible.

Cheers
Alex

giammy92 · April 22, 2016, 08:37

And do you think that bc for k and nut that I've set are corrected?

giammy92 · April 22, 2016, 08:57

Now i'm trying with my current bc that i've typed at the beginning of thread but a progressive increase of divergence order:

beginning

div(phi,U) bounded Gauss linearUpwind grad(U)
div(phi,k) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind

after stabilization:

div(phi,U) bounded Gauss linearUpwind grad(U)
div(phi,k) Gauss linearUpwind default
div(phi,omega) Gauss linearUpwind default

after stabilization:

div(phi,U) Gauss linear
div(phi,k) Gauss linearUpwind default
div(phi,omega) Gauss linearUpwind default

What do you think of this approach?
A doubt...but word bounded must precede Gauss even in other divSchemes?

giammy92 · April 22, 2016, 09:13

I have a problem when I switch from:

div(phi,k) bounded Gauss upwind ----> bounded Gauss linearUpwind default
div(phi,omega) bounded Gauss upwind ----> bounded Gauss linearUpwind default

my force coeffs have big oscillations. How can i improve my results with another divSchemes?
What do you think about bounded Gauss limitedLinear 1 for k and omega?

giammy92 · April 24, 2016, 13:40

Checking geometry...
Overall domain bounding box (-21.836 -21.836 -0.617615) (21.836 21.836 0.617615)
Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
Mesh has 2 solution (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-6.95824e-18 1.76479e-18 1.07587e-19) OK.
Max cell openness = 2.66696e-15 OK.
Max aspect ratio = 112.064 OK.
Minimum face area = 2.31703e-11. Maximum face area = 0.734078. Face area magnitudes OK.
Min volume = 2.86207e-11. Max volume = 0.159436. Total volume = 1849.45. Cell volumes OK.
Mesh non-orthogonality Max: 88.3385 average: 6.90415
*Number of severely non-orthogonal (> 70 degrees) faces: 171.
Non-orthogonality check OK.
<<Writing 171 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.42922 OK.
Coupled point location match (average 0) OK.

Mesh OK.

giammy92 · April 24, 2016, 13:44

particulars of structured mesh near wall

giammy92 · April 24, 2016, 20:05

forces
{
type forces;

functionObjectLibs ( "libforces.so" );

outputControl timeStep;
timeInterval 1;

log yes;

patches ( "TRAILING_EDGE" "SUCTION_SIDE" "PRESSURE_SIDE" );
pName p;
UName U;
rhoName rhoInf; // Indicates incompressible
log true;
rhoInf 1.22568; // Redundant for incompressible

CofR (0 0 0); // Rotation around centre line of propeller
pitchAxis (0 0 1);
}

forces
{
type forceCoeffs;

functionObjectLibs ( "libforces.so" );

outputControl timeStep;
timeInterval 1;

log yes;

patches ( "TRAILING_EDGE" "SUCTION_SIDE" "PRESSURE_SIDE" );
liftDir (-0.22495 0.97437 0);
dragDir (0.97437 0.22495 0);
magUInf 41.511;
lRef 0.5459;
Aref 0.5459;
}

I have a doubt about the value to give in rhoInf in forces file. I have set real rho of air at 288 K and p=101325 Pa that is rho= 1.22568 kg/m^3.
But sometimes i have seen rho set to 1.
In my case is right set 1 or real value? Why?

giammy92 · April 26, 2016, 07:21

What do you recommend me to correct influence of non orthogonal elements around my airfoil???

Kina · April 26, 2016, 15:49

I usually set my rho to 1.205 but that shouldn't be the cause of your problem. Estimating drag values is a problem closely connected to many variables. You are using a fully turbulent model while the flow is transitional in reality. Have you tried setting up a k-kl-omega model?
Do you have the ability to create a new mesh?

giammy92 · April 26, 2016, 16:31

no, also if i don't use a transitional model my value of Cd are wrong compared with a precedent thesis work performed with Fluent, that with same turbulence model k-w SST, gives a value of Cd around 0.02-0.03. However this Fluent simulation uses a grid fully structured, while i'm using a mix-grid, how you can see from pictures. My grid is been imported from Fluent and it is been used in another thesis work, performed with Transitional SST that gives about same Cd. Anyway i can't modify mesh to remove non orthogonal faces, at maximum i would try to use topoSet and subsetMesh to remove non orthogonal faces but i can't set topoSetDict

Sorry i don't know what i can do to resolve this problem

Kina · April 26, 2016, 16:44

Does the thesis paper specifically say that there was no transition model used?
As far as I know, the SST in fluent works with the gamma-ReThetat transition.

giammy92 · April 26, 2016, 17:12

Yes, simulation with k-w SST is been performed without tansition. This is been done with Transition SST model

erlofg · April 28, 2016, 04:16

Even if the flow would be fully turbulent in the experiment, as it is in your simulation, the actual drag coefficient will also depend on the turbulent intensity. For higher levels of TI at fixed Re, the drag coefficient will drop according to Swallwell et al. 2001 (“The Effect of turbulence Intensity on Stall of the NACA 0021 Aerofoil,”).

So you would have to match your TI to that of the experimental data, which is rarely specified, to get a perfect agreement. The difference in Cd may be hundreds of percents!

/ Erik

giammy92 · April 28, 2016, 08:16

In the thesis paper is specified Tl that is of 0.1%
I have also tried with k-Omega LowRe that should works with same damping function used in Fluent but i have same results of standard K-Omega SST

In particular when i set to wall's bc omegawallfuntion i have a very high of Cl 1.578 against 1.2 of experimental data but Cd is very good 0.0258 according to exp data.
Instead when i set omega to fixed value 1e-12, how suggested for meshes that haven't need of wall functions, i have a good Cl of about 1.2 but Cd is very high of 0.07.
I don't know if my problem is turbulence model or my mesh with high non orthogonality, but maybe mesh is not the problem since i have at least one result good.
I think that i will try with k-kl-omega but i would know which value of kt and kl set.
Kt should be same of my k because that is turbulent kinetic energy? But about of kl that is laminar kinetic energy what bc i have to set at wall and far field?

April 21, 2016, 13:34	Cd too high with k-w SST	#1
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	Dear all, I'm performing a thesis in which i have to calculated force coefficients of an airfoil 2 D invested by a flux inclined of 13 deg compared to chord. I want use k-w SST and simpleFoam. I report you my 0 file: -K dimensions [0 2 -2 0 0 0 0]; internalField uniform 0.0025847; boundaryField { TRAILING_EDGE { type fixedValue; value uniform 1e-12; } SUCTION_SIDE { type fixedValue; value uniform 1e-12; } FAR_FIELD { type turbulentIntensityKineticEnergyInlet; intensity 0.001; value uniform 0.0025847; } PRESSURE_SIDE { type fixedValue; value uniform 1e-12; } frontAndBackPlanes { type empty; } } -NUT dimensions [0 2 -1 0 0 0 0]; internalField uniform 1.4599e-6; boundaryField { TRAILING_EDGE { type nutLowReWallFunction; value uniform 0; } SUCTION_SIDE { type nutLowReWallFunction; value uniform 0; } FAR_FIELD { type calculated; value uniform 1.4599e-6; } PRESSURE_SIDE { type nutLowReWallFunction; value uniform 0; } frontAndBackPlanes { type empty; } } -OMEGA dimensions [0 0 -1 0 0 0 0]; internalField uniform 1770.43; boundaryField { TRAILING_EDGE { type fixedValue; value uniform 1e-12; } SUCTION_SIDE { type fixedValue; value uniform 1e-12; } FAR_FIELD { type turbulentMixingLengthFrequencyInlet; mixingLength 5.2428e-5; value uniform 1770.43; } PRESSURE_SIDE { type fixedValue; value uniform 1e-12; } frontAndBack { type empty; } } -P dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { TRAILING_EDGE { type zeroGradient; } SUCTION_SIDE { type zeroGradient; } FAR_FIELD { type freestreamPressure; } PRESSURE_SIDE { type zeroGradient; } frontAndBackPlanes { type empty; } } -U dimensions [0 1 -1 0 0 0 0]; internalField uniform (40.447 9.338 0); // (41.511cos13 41.511sin13) boundaryField { TRAILING_EDGE { type fixedValue; value uniform (0 0 0); } SUCTION_SIDE { type fixedValue; value uniform (0 0 0); } FAR_FIELD { type freestream; freestreamValue uniform (40.447 9.338 0); } PRESSURE_SIDE { type fixedValue; value uniform (0 0 0); } frontAndBackPlanes { type empty; } } My mesh is enogh refine to wall, i have y+ about 1 or less, so i don't use wall function and I've used for k, omega and nut the bc suggested for a mesh with y+<5, by this site http://www.dicat.unige.it/guerrero/o...turbulence.pdf I've achieved an acceptable value of Cl of about 1.17 against 1.2 of experimental data, but my Cd is far away, 0.07 against about 0.02 of exp. data. My supervisor suggests me to change wall's bc for k and omega without use wall functions...but i don't have any idea of which kind of bc i can use Do you recommend me change other bc? Please help me, this problem is taking me a long time, I want graduate quicky!!!

April 24, 2016, 20:05	forces and force coefficients	#13
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	forces { type forces; functionObjectLibs ( "libforces.so" ); outputControl timeStep; timeInterval 1; log yes; patches ( "TRAILING_EDGE" "SUCTION_SIDE" "PRESSURE_SIDE" ); pName p; UName U; rhoName rhoInf; // Indicates incompressible log true; rhoInf 1.22568; // Redundant for incompressible CofR (0 0 0); // Rotation around centre line of propeller pitchAxis (0 0 1); } forces { type forceCoeffs; functionObjectLibs ( "libforces.so" ); outputControl timeStep; timeInterval 1; log yes; patches ( "TRAILING_EDGE" "SUCTION_SIDE" "PRESSURE_SIDE" ); liftDir (-0.22495 0.97437 0); dragDir (0.97437 0.22495 0); magUInf 41.511; lRef 0.5459; Aref 0.5459; } I have a doubt about the value to give in rhoInf in forces file. I have set real rho of air at 288 K and p=101325 Pa that is rho= 1.22568 kg/m^3. But sometimes i have seen rho set to 1. In my case is right set 1 or real value? Why?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Drag force coefficient too high for a flow past a cylinder using komega sst	Scabbard	OpenFOAM Running, Solving & CFD	37	March 21, 2016 17:16
k-omega SST SAS High Wavenumber Damping Limiter	PonchO	OpenFOAM Programming & Development	5	March 21, 2016 13:01
At high Y+ values does the K Omega SST model just behave like the K Epsilon model?	JuPa	CFX	0	December 22, 2015 07:44
High curvature 90 degree bend using SST, eddy viscosity drop??	tinab0binuh	Main CFD Forum	0	August 22, 2014 18:26
Multicomponent fluid	Andrea	CFX	2	October 11, 2004 06:12

April 21, 2016, 13:47		#2
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	fv Schemes ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss GammaV 0.2; div(phi,k) bounded Gauss limitedLinear 1; div(phi,omega) bounded Gauss limitedLinear 1; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } fv Solution solvers { p { solver GAMG; tolerance 1e-7; relTol 0; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; nSweeps 1; tolerance 1e-08; relTol 0; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; residualControl { p 1e-5; U 1e-5; k 1e-5; omega 1e-5; } } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.7; omega 0.7; } }

April 22, 2016, 03:54		#3
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Do you know from your physical conditions that the boundary layer is fully turbulent? kOmegaSST in OF models fully turbulent conditions. Maybe you have to implement a transition model. Also, try to change your scheme for div(phi,U) as it affects the drag value by a large percentage. For my problem, drag reduces by more than 10% with "bounded linear" instead of "bounded linearUpwindV grad(U)". Cheers Alex

April 22, 2016, 06:38		#4
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	thank you for your reply Kina Yes my boundary layer is fully devoleped, i have Re = 1.5 e6. Furthermore my supervisor suggests me to try with calculated k and omega to wall. Is it reasonable?

April 22, 2016, 07:13		#5
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Your omega values are kinda weird. I suggest you calculate your omega with the second omega equation given here: http://www.cfd-online.com/Wiki/Turbu...ary_conditions set your omega to 10^8 at walls. yours is too small as omega theoretically rises to infinity at walls. Cheers Alex

April 22, 2016, 07:45		#6
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	but which type of bc for omega? fixedValue or calculated?

April 22, 2016, 08:28		#7
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	fixedValue. I wouldn't set k or omega to calculated - I am not even sure if that's possible. Cheers Alex

April 22, 2016, 08:37		#8
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	And do you think that bc for k and nut that I've set are corrected?

April 22, 2016, 08:57		#9
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	Now i'm trying with my current bc that i've typed at the beginning of thread but a progressive increase of divergence order: beginning div(phi,U) bounded Gauss linearUpwind grad(U) div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind after stabilization: div(phi,U) bounded Gauss linearUpwind grad(U) div(phi,k) Gauss linearUpwind default div(phi,omega) Gauss linearUpwind default after stabilization: div(phi,U) Gauss linear div(phi,k) Gauss linearUpwind default div(phi,omega) Gauss linearUpwind default What do you think of this approach? A doubt...but word bounded must precede Gauss even in other divSchemes?

April 22, 2016, 09:13		#10
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	I have a problem when I switch from: div(phi,k) bounded Gauss upwind ----> bounded Gauss linearUpwind default div(phi,omega) bounded Gauss upwind ----> bounded Gauss linearUpwind default my force coeffs have big oscillations. How can i improve my results with another divSchemes? What do you think about bounded Gauss limitedLinear 1 for k and omega?

April 26, 2016, 15:49		#15
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	I usually set my rho to 1.205 but that shouldn't be the cause of your problem. Estimating drag values is a problem closely connected to many variables. You are using a fully turbulent model while the flow is transitional in reality. Have you tried setting up a k-kl-omega model? Do you have the ability to create a new mesh?

April 26, 2016, 16:31		#16
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	no, also if i don't use a transitional model my value of Cd are wrong compared with a precedent thesis work performed with Fluent, that with same turbulence model k-w SST, gives a value of Cd around 0.02-0.03. However this Fluent simulation uses a grid fully structured, while i'm using a mix-grid, how you can see from pictures. My grid is been imported from Fluent and it is been used in another thesis work, performed with Transitional SST that gives about same Cd. Anyway i can't modify mesh to remove non orthogonal faces, at maximum i would try to use topoSet and subsetMesh to remove non orthogonal faces but i can't set topoSetDict Sorry i don't know what i can do to resolve this problem

April 26, 2016, 16:44		#17
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Does the thesis paper specifically say that there was no transition model used? As far as I know, the SST in fluent works with the gamma-ReThetat transition.

April 26, 2016, 17:12		#18
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	Yes, simulation with k-w SST is been performed without tansition. This is been done with Transition SST model

April 28, 2016, 04:16		#19
erlofg New Member Erik Löfgren Join Date: Feb 2015 Location: Umeå, Sweden Posts: 9 Rep Power: 11	Even if the flow would be fully turbulent in the experiment, as it is in your simulation, the actual drag coefficient will also depend on the turbulent intensity. For higher levels of TI at fixed Re, the drag coefficient will drop according to Swallwell et al. 2001 (“The Effect of turbulence Intensity on Stall of the NACA 0021 Aerofoil,”). So you would have to match your TI to that of the experimental data, which is rarely specified, to get a perfect agreement. The difference in Cd may be hundreds of percents! / Erik

April 28, 2016, 08:16		#20
giammy92 Senior Member Join Date: Mar 2016 Posts: 133 Rep Power: 10	In the thesis paper is specified Tl that is of 0.1% I have also tried with k-Omega LowRe that should works with same damping function used in Fluent but i have same results of standard K-Omega SST In particular when i set to wall's bc omegawallfuntion i have a very high of Cl 1.578 against 1.2 of experimental data but Cd is very good 0.0258 according to exp data. Instead when i set omega to fixed value 1e-12, how suggested for meshes that haven't need of wall functions, i have a good Cl of about 1.2 but Cd is very high of 0.07. I don't know if my problem is turbulence model or my mesh with high non orthogonality, but maybe mesh is not the problem since i have at least one result good. I think that i will try with k-kl-omega but i would know which value of kt and kl set. Kt should be same of my k because that is turbulent kinetic energy? But about of kl that is laminar kinetic energy what bc i have to set at wall and far field?